Revision as of 02:53, 18 November 2010

Hoi Bridge

Very nice start. I added the coordinates of the point P1 .. P16. Did you give all coordinate by hand?

Regarding the local stresses SIXX, SIYY etc: did you take the SUP layer?

kees

Hi Kees, our's tutorial grows very rapidly :D
i used your's files from forum,
for SIXX,SIYY,SIXY i used: resuSUP_SIGM_NOEU_DEPL__________ -> scalar map
where can I choose the SUP layer?

- there was error in bc, correct are: Lleft: (DX=0.0,DY=0.0,DZ=0.0); Lright: (DZ=0.0); Ltop,Lbot: free
- i fixed it in:

• Create two groups for boundary conditions
• Reactions

- You are right, area 73.3 is correct

• my ideas:
  

1. export list of ReactionForces at nodes of Nleft and Nright group to txt file,
2. export ReactionForces at nodes of Nleft and Nright group to to med file and make scalar maps or vector
3. what is the best way to get max displacement DZ? Directly from Deformed shape = 0,0292?

Growing:
Is it like the economy: the more we grow the better? Or do we need to watch quality? ;-)
BC:
So the BCs given in the wiki are correct now, are not they?

Selection of layer is performed in the CALC_ELEM command:
To calculate displacements (no need for selecting a layer here though):

resu=CALC_ELEM(reuse=resu,
            MODELE=modmod,
            CHAM_MATER=material,
            RESULTAT=resu,
            REPE_COQUE=_F(NIVE_COUCHE='SUP',),#this determines layer for the EQUIvalent stresses 'EQUI_ELNO_SIGM'
            OPTION=('SIGM_ELNO_DEPL',),);      #includes data for 'DEPL' and 'SIGM_NOEU_DEPL'

I use a new field to get the results at layer SUP:

resuSUP=CALC_ELEM(MODELE=modmod,
                CHAM_MATER=material,
                RESULTAT=resu,
                REPE_COQUE=_F(NIVE_COUCHE='SUP',), ## select outer layer here
                OPTION=('SIGM_ELNO_DEPL','EQUI_ELNO_SIGM',),);

you can also add e.g:

resuINF=CALC_ELEM(MODELE=modmod,
                CHAM_MATER=material,
                RESULTAT=resu,
                REPE_COQUE=_F(NIVE_COUCHE='INF',),  ## select inner layer here
                OPTION=('SIGM_ELNO_DEPL','EQUI_ELNO_SIGM',),);

and add them in the IMPR_RESU command. Do the same for 'MOY' for central layer if needed.

About reaction forces:

• 1: I added the table command: you get the total reaction forces. But I know I used a parameter that gives the requested field at all nodes. Need to search a bit.
• 2: correct: look at the end of the contribution. But The strange thing is that the midside node have large positive reactions whereas the corner nodes have negative reactions. Might be correct though (????), but need to look at it. The diameter of the nodes indicate value of reaction forces.
• I normally look at the shape and see what is the maximum value. In Salome 4.x the maximum and minimum values were displayed in the scale, but now these values seems to be rounded. The is an option to extract the min/max displacements/stress/strain values. But I never used it, so need the search for it.

For now my command file: Media:kw_shell5.zip

> Is it like the economy: the more we grow the better? Or do we need to watch quality? ;-) I think that more is better, Specially better than none :)

For now, I think the most important is to sync our command files, mesh and all other stuf.
We have to work at the same files.
I will check and update Your command file: Media:kw_shell5.zip with mine.

I see that in your command file:
- we have different materials (my's: concrete, your's:steel)
- we have different bc (my's: Lleft,Lright your's:Ltop,Lbot)

I check this and update your's file.

STRANGE ERROR

I try to load your's file [from Media:kw_shell5.zip] to CAELinux 2009 Eficas V1.15 and get Error

What software are You using?
I use CAELinux 2009 (Eficas V1.15) for computing ASTER files.
Is it obsolete?

I have Salome 5.1.3 but without integrated ASTER (pre&post procesing).

shell.mess:

...
==========================================
JDC.py : ERREUR DE COMPILATION DANS ACCAS - INTERRUPTION
>> JDC.py : DEBUT RAPPORT
CR phase d'initialisation
  !!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!
  ! Compilation impossible :   File "fort.1", line 156 !
  !      TITRE='[Reaction] Nodal Forces',);            !
  !           ^                                        !
  !  SyntaxError: invalid syntax                       !
  !!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!
fin CR phase d'initialisation

>> JDC.py : FIN RAPPORT
EXECUTION_CODE_ASTER_EXIT_13342=1

<F>_ABNORMAL_ABORT  exit code = 1

• I manually updated Your file (bc and material)

Comm file:Media:Shell7.comm.zip

Hoi Bridge

Sorry for that error. I have the same. I replaced the table extraction manually with a different piece later. I donot understand what is wrong in this part though.
I use Eficas 1.8.0 sometimes (seldom), to edit my comm file. Most of the time I edit manually.
CODE_ASTER -- VERSION DE DEVELOPPEMENT 10.01.09

About the maximum displacement: I guess your value is correct:
3. what is the best way to get max displacement DZ? Directly from Deformed shape = 0,0292?

The maximum displacement Code Aster reports is 0.0291....

* INTITULE         * RESU     * NOM_CHAM         * NUME_ORDRE   * EXTREMA  * NOEUD    * CMP      * VALE        
* displacements dz * resu     * DEPL             *            1 * MAX      * N115     * DZ       *  2.91659E-02

New command file: Comm file:Media:Shell8.comm.zip

Oeps, sorry, I need to mention that the pressures have changed sign. This is just nicer in the reaction forces, diameter indicating the reaction forces. I donot know whether there is a nicer way to show the reaction forces.

I use coarser mesh. Min/max of stresses added. Fun.

Hoi,

Can You upload here Your's comm file with all table commands?
Where can I find results tables? In which file?
When I click Solve Aster Case in CAELinux several screens of data flashes at console and I cannot find tables.

I make deformations and reactions graphics:

but it looks strange to me...

why reactions at edge are: bigger, smaler, bigger, smaler, bigger, smaler...
closest reactions should be equal Regs

Hoi Bridge

Very nice figure you produce! How do you create these reaction forces? Vector representation?
Reaction forces: yes, that is my worry also: smaller at the corner nodes of the triangles, larger reactions at the midside nodes. But it still *might* be correct and and can be related to the way the virtual forces are determined on the triangle. But I would expect a more equal distribution. And of course the reaction forces at each node depend on the fineness of the mesh: the larger the elements the larger the reaction force at each node (number of supporting nodes * average of reaction force --> total reaction force. So we need to look at distributed reaction force: force per unit length?
The tables are on unit 26. So you have to define a additional file in ASTK. The unit number is defined at the IMPR_TABLE command.
I have been testing a bit with these table. I will upload shell11.comm and shell12.com. There is a bit of Python involved to shorten the command. I hope I didnot make it too complicated.
Comm file:Media:kw_shell11_12.zip

Some result of the file 'reaction.txt':

* NOM_CHAM         * DZ           * MOMENT_X     * MOMENT_Y     * EXTREMA  * NOEUD    * CMP      * VALE        
* REAC_NODA        *  5.04036E+06 * -            * -            * -        * -        * -        * -           
* REAC_NODA        * -            *  3.06316E+07 * -3.53025E+07 * -        * -        * -        * -           
* FORC_NODA        *  4.90339E+06 * -            * -            * -        * -        * -        * -           

* EQUI_NOEU_SIGM   * -            * -            * -            * MAX      * N290     * VMIS     *  6.93261E+06
* EQUI_NOEU_SIGM   * -            * -            * -            * MIN      * N271     * VMIS     *  4.74148E+05
* EQUI_NOEU_SIGM   * -            * -            * -            * MAX_ABS  * N290     * VMIS     *  6.93261E+06
* EQUI_NOEU_SIGM   * -            * -            * -            * MIN_ABS  * N271     * VMIS     *  4.74148E+05
* EQUI_NOEU_SIGM   * -            * -            * -            * MAX      * N290     * TRESCA   *  7.65875E+06
* EQUI_NOEU_SIGM   * -            * -            * -            * MIN      * N271     * TRESCA   *  5.46807E+05
* EQUI_NOEU_SIGM   * -            * -            * -            * MAX_ABS  * N290     * TRESCA   *  7.65875E+06
* EQUI_NOEU_SIGM   * -            * -            * -            * MIN_ABS  * N271     * TRESCA   *  5.46807E+05
* EQUI_NOEU_SIGM   * -            * -            * -            * MAX      * N271     * PRIN_1   * -1.99226E+05
* EQUI_NOEU_SIGM   * -            * -            * -            * MIN      * N182     * PRIN_1   * -3.00400E+06
* EQUI_NOEU_SIGM   * -            * -            * -            * MAX_ABS  * N182     * PRIN_1   *  3.00400E+06
* EQUI_NOEU_SIGM   * -            * -            * -            * MIN_ABS  * N271     * PRIN_1   *  1.99226E+05
* EQUI_NOEU_SIGM   * -            * -            * -            * MAX      * N152     * PRIN_2   *  5.90883E+05
* EQUI_NOEU_SIGM   * -            * -            * -            * MIN      * N48      * PRIN_2   * -1.02255E+06
* EQUI_NOEU_SIGM   * -            * -            * -            * MAX_ABS  * N48      * PRIN_2   *  1.02255E+06
* EQUI_NOEU_SIGM   * -            * -            * -            * MIN_ABS  * N50      * PRIN_2   *  1.86548E+04
* EQUI_NOEU_SIGM   * -            * -            * -            * MAX      * N290     * PRIN_3   *  5.17802E+06
* EQUI_NOEU_SIGM   * -            * -            * -            * MIN      * N271     * PRIN_3   *  3.47581E+05
* EQUI_NOEU_SIGM   * -            * -            * -            * MAX_ABS  * N290     * PRIN_3   *  5.17802E+06
* EQUI_NOEU_SIGM   * -            * -            * -            * MIN_ABS  * N271     * PRIN_3   *  3.47581E+05

* SIGM_NOEU_DEPL   * -            * -            * -            * MAX      * N290     * SIXX     *  1.16286E+06
* SIGM_NOEU_DEPL   * -            * -            * -            * MIN      * N182     * SIXX     * -7.60697E+05
* SIGM_NOEU_DEPL   * -            * -            * -            * MAX_ABS  * N290     * SIXX     *  1.16286E+06
* SIGM_NOEU_DEPL   * -            * -            * -            * MIN_ABS  * N31      * SIXX     *  4.34115E+04
* SIGM_NOEU_DEPL   * -            * -            * -            * MAX      * N290     * SIYY     *  8.73871E+05
* SIGM_NOEU_DEPL   * -            * -            * -            * MIN      * N208     * SIYY     * -6.88356E+05
* SIGM_NOEU_DEPL   * -            * -            * -            * MAX_ABS  * N290     * SIYY     *  8.73871E+05
* SIGM_NOEU_DEPL   * -            * -            * -            * MIN_ABS  * N182     * SIYY     *  5.08765E+04
* SIGM_NOEU_DEPL   * -            * -            * -            * MAX      * N182     * SIXY     *  1.88556E+06
* SIGM_NOEU_DEPL   * -            * -            * -            * MIN      * N81      * SIXY     * -9.99157E+05
* SIGM_NOEU_DEPL   * -            * -            * -            * MAX_ABS  * N182     * SIXY     *  1.88556E+06
* SIGM_NOEU_DEPL   * -            * -            * -            * MIN_ABS  * N271     * SIXY     *  5.56380E+04
* SIGM_NOEU_DEPL   * -            * -            * -            * MAX      * N290     * SIXZ     *  2.55082E+06
* SIGM_NOEU_DEPL   * -            * -            * -            * MIN      * N152     * SIXZ     * -1.08203E+06
* SIGM_NOEU_DEPL   * -            * -            * -            * MAX_ABS  * N290     * SIXZ     *  2.55082E+06
* SIGM_NOEU_DEPL   * -            * -            * -            * MIN_ABS  * N182     * SIXZ     *  9.22192E+04
* SIGM_NOEU_DEPL   * -            * -            * -            * MAX      * N48      * SIYZ     *  2.54240E+06
* SIGM_NOEU_DEPL   * -            * -            * -            * MIN      * N9       * SIYZ     * -2.60463E+05
* SIGM_NOEU_DEPL   * -            * -            * -            * MAX_ABS  * N48      * SIYZ     *  2.54240E+06
* SIGM_NOEU_DEPL   * -            * -            * -            * MIN_ABS  * N271     * SIYZ     *  2.61977E+03

Yes, I used Vector gfx to show reaction forces, it's the best way.
I'm thinking about nodal reactions - why they are smaller....
btw, nice work with ASTK tutorial, very usefull :D
now i'm trying to compile lastest aster-code on my desktop (instead using livedvd)

Hoi Bridge
1) Can you update the part regarding the display of the reaction/nodal forces in the content page? The arrows on the nodes are much better than the thickness of the balls.
2) Should we add a new page on extracting the maximum and resulting quantities of stresses and forces? Or do we leave it as is and add some details here?

Hoi Kees ok! I update the part regarding the display of the reaction/nodal forces in the content page.
>Should we add a new page on extracting the maximum and resulting quantities of stresses and forces?
> Or do we leave it as is and add some details here?
We should add a new page, discussion here is a bit chaotic :D
Im trying to create hexahedralization mesh but there occurs error and I have no idea how to fix it.


hexahedralization mesh works when there in no partitions.
I will check later if hexahedralization mesh gives the same results reactions (big and small ones).
my ideas to add to this tutorial:

• find principal stresses, principal directions (important when we use concrete)
• make graph of ie. Mxx (Mxx=Sixx*Wx)

Regards :D

The hexahedron mesh needs four edges: each two opposite the other one. From one side mesh lines go to opposite edge. You can use more edges, but then you need to combine two or more. So lines from one edge go to selected opposite edges. I have seen it on Salome site, but at this moment I need once again search and look for it. Come back on this later. And regarding the isle in the centre, I donot know whether you can circumvent that. About retrieval of stresses and forces we can add a new directory. Will do that.

five edges for quadrangle (from Salome site):
http://erwan.adam.free.fr/salome/scripts/Mesh_on_5_edges_00.png
http://www.salome-platform.org/forum/forum_11/thread_2893

You can see what is going on with this file (load script or cntrl T in salome object browser, also from Salome site):
Comm file:Media:mesh_hexahedron.py.zip

Most of the table part has been moved to http://www.caelinux.org/wiki/index.php/Contrib:KeesWouters/shell/tables

baai baai - kees

>== hexahedron mesh ==

I go my way :D and create hexahedron mesh !! <br>

• Mesh i good, and have groups.

<br> <br> <br> <br> <br> <br> Media:Mesh-q.med.zip <br> <br>

• ASTER ERROR - I have no idea what is wrong :(

                                 -- CODE_ASTER -- VERSION DE DEVELOPPEMENT STABILISEE 10.01    --
                                                        VERSION SEQUENTIELLE
                                                  COPYRIGHT  EDF-R&D 1991 - 2009
                                              EXECUTION DU : VE-19-MARS-2010 19:14:55
                                               NB MAX PROC OpenMP:   1             
                                                    SYSTEME : LINUX           
                                                      CPU : X86_64          
  
  !---------------------------------------------------------------------------------------------------------------------------------!
  ! <EXCEPTION> <MODELISA6_96>                                                                                                      !
  !                                                                                                                                 !
  !                                                                                                                                 !
  !  les 60 mailles imprim�es ci-dessus n'appartiennent pas au mod�le et pourtant elles ont ete affect�es dans le mot-cl� facteur : !
  ! FORCE_COQUE                                                                                                                     !
  !                                                                                                                                 !
  !                                                                                                                                 !
  !                                                                                                                                 !
  !                                                                                                                                 !
  !---------------------------------------------------------------------------------------------------------------------------------!

<nowiki><S> ERREUR UTILISATEUR RECUPEREE PAR LE SUPERVISEUR</nowiki>
<nowiki><I> <FIN> FERMETURE DE LA BASE "GLOBALE" EFFECTUEE.</nowiki>
<nowiki><I> <FIN> ARRET NORMAL DANS "FIN" PAR APPEL A "JEFINI".</nowiki>
<nowiki><I>       FERMETURE DES BASES EFFECTUEE

</nowiki>

Hoi Bridge

Because you have both triangles and quads now, you need to modify:

#meshmod=CREA_MAILLAGE(MAILLAGE=meshinit,
#                      MODI_MAILLE=_F(TOUT='OUI',
#                                     OPTION='TRIA6_7',),);

meshmod=CREA_MAILLAGE(MAILLAGE=meshinit,
                     MODI_MAILLE=(_F(TOUT='OUI',OPTION='TRIA6_7',),
                                  _F(TOUT='OUI',OPTION='QUAD8_9',),),);

and then it runs. Here it does.

And, can you explain how you made this quad mesh? Very much interested.

tot ziens - kees

Okie :D I'll make hexa hedra tutorial :D

hexahedron mesh updated!

Hi,
I uploaded graphics and wrote few words about hexahedron mesh :)
Have fun,
Regards

Hoi Bridge
Nice to see the way of working for hexa mesh.
Do we need to add more topics are details?
Maybe definition of local stresses SIXX, ...?
kind regards - kees

I'm not sure how much detailled this tutorial should be.

Have You idea how to:

• find principal stresses, principal directions and make graph (important when we use concrete)
  
• make graph of Mxx (Mxx=Sixx*Wx), Myy (Myy=Siyy*Wy)
  

At the end it will be nice compare triangle and hexa mesh:

• (compare forces, reactions and find out which is better)
  

From my experience with 3d mesh i think hexa is better.
So i spent much time to get 2d hexa mesh working.
Regards

Regarding principal stresses:
the values themselves are readily available. The direction I am not sure how to obtain these at the moment.
graph of Mxx and Myy: my guess is that you have to derive them from Si_ab and the thickness of the plate (W_ab). But I have not looked at this problem before. Maybe we should ask in the forum (CAELinux/Code Aster).
Compare reactions, forces and displacements between different meshes can be done (I have done that before: [comparsion tria - quad mesh]) and indeed quadrangles are better, although for quadratic elements the difference is not too large. The difference between linear and quadratic elements is very large indeed. This is valid for solid elements, maybe we can compare between shell elements.